[smarko77]

Hello,

I have CNC machine which I am using for woodworking and 3d carving. It has 8Nm stepper motors for 3 axis (two motors for Y axis) and 2kw spindle. I am using Mach3 for machine operations and Vectric Aspire for file preparation.

Machine is calibrated and is working great, but I have one strange issue when i am doing 3d carving.




All the details looks great, but in some areas I see carve marks which are 2-3mm tick and much ticker then bit I was using (0.75mm tapered ball nose bit, 8% stepover. Interesting is that these marks are seen on areas where there is enough room for machine to accelerate and then needs to change z axis after that. Marks are gone on areas where machine has to slow down where there are more complex details. I am attaching pictures. I tried both X and Y axis to check if I will get different result, but it is the same. Speedrate is 3000mm/min and plunge rate is 2000mm/min.

For the love of God I cannot understand why is this happening. Anyone?

Marko

[peteeng]

Hello Marko - Are these being carved from stl files? If so the toolpath result is dependent on mesh size so you may have to decrease the mesh size to improve the local details. If you can look at the toolpath in Aspire in these areas that may give you some clues. There is also the issue of the accuracy settings in M3. I'm not a M3 user so can't guide you on these but they can be important for detailed work. Peter

[RaderSidetrack]

Marko did post photos, but they did not transfer to CNCZone due to server issues. You can see the photos here: https://en.industryarena.com/forum/s...d.php?t=478001

[routalot]

It might be the harmonics of the machine structure or it might be related to the varying of the power fed to the motor controllers as an additional stepper needs to move.Could you provide more details of the machine construction?An assembly of extrusions will have more of a tendency to vibrate than a welded structure of hefty steel and an all cast iron gantry would be better again.

Are you using that tiny cutter for the entire job?It would take forever and leave lots of tiny cusps.I try to use the largest diameter cutter for the majority of the surface and then use an additional layer (or several layers) to define regions where there is no option other than something much smaller.The result of using the largest practical tool diameter for each region is that the cutting time is greatly reduced and the cusps that remain are a much smaller proportion of the tool diameter.With Vectric software there is the facility to select geometry to limit the cutting zone and you may find that you save a lot of time and reduce the amount of hand finishing.

[smarko77]

Thank you everybody for trying to help. I will try to answer the best I can

Yes, it is being carved from STL file which I imported into Aspire. STL file is already created, so I didn't create it myself. I just simulated my tool paths in Aspire and I also marked areas with errors with blue. What is weird, but also a possible clue is that is presented in specific area between the letters (marked with blue).
About CNC machine. I built it by myself. Gantry is built from solid steel and it is very heavy, same as machine base. Everything is welded and very rigid. I could take some pictured of the machine if this would help.

I used 6mm bit for roughing job and then whole finishing toolpath is done with 0.75mm tappered ballnose bit with 8% stepover. Yes, it takes a very long time (6-7 hours in this case for finishing toolpath).

[smarko77]

Little more about machine.

I am using 4 stepper motors, 2 on Y axis and one for X and Y axis. These are Nema 34 Stepper motors, 8Nm each. Each has It's on stepper driver, I believe it is HSS86. Each has separate power supply (400w each).
I am using cheap Mach3 serial port card. I am attaching few pictures.

[peteeng]

sorry your images are not opening. A clue is that some stl "surfaces" have recurves (hollows) in them and it depends on how Aspire interpolates between edges on how the toolpath works. Not being an aspire user but have a look and see if it has some sort of smoothing function. This will improve the stl "surface" before you toolpath it. Peter

an stl "surface" is not a geometric surface but is made up of many many triangular elements that infer a "surface" called a mesh. If the mesh has small hollows that are smaller than your tool the CAM has to interpolate across the apparent gap and this can lead to various toolpath issues. Or the tool is capable of diving into the hollow but the motion controller can't so it shortcuts the feature... A few things to work thru.

[smarko77]

Don't know why you cannot see images

I will try to upload it on this link:

https://postimg.cc/gallery/2jrsq7k

[routalot]

The images show a solid machine.I would still suggest that you add a layer for some boundaries and keep the tiny finishing cutter from having to remove material from those elliptical egg like features as the larger cutter would leave a nicer finish and there may be other areas where perhaps boundaries could be used to allow a flat bottom cutter to remove material.Which might be a chore if you don't have a toolchanger.

I only have experience of Vcarve from Vectric and can't comment on the range of file types that can be imported into Aspire.What might be worth investigating is whether Meshlab could be a useful tool for cleaning up the areas that are causing problems.i have a copy on my computer but since I don’t import .stl files,I have never needed to use it.It doesn't cost anything,so there is only lost time as a downside.I have to say that my limited experience of 3d machining with Vcarve would lead me to believe that Aspire ought to be better or there is little reason to upgrade.

[awerby]

That's the effect of a rastering cut going over steep areas. It's not happening because your STL mesh is too coarse. On a relatively flat surface, the cusps will blend into one another, but as it becomes steeper, it's cutting more with the side of the tool, and the geometry of the cut changes, since the cuts are spaced further apart vertically. It can help to overlay a different kind of toolpath and run it again, so if this was parallel passes at a certain horizontal distance from one another, the next one can be a "waterline" strategy, where the cuts are a certain distance apart vertically. Another thing you can do is outline each letter with a cleanup cut, which is more tedious to set up, but will run a lot faster.

[routalot]

There is one other factor which we haven't mentioned;the slenderness of the cutter.With a diameter of 0.75mm and some comparatively deep features to traverse,it may well be that the projecting length of the cutter is several multiples of the diameter and perhaps prone to flexing as the proportion of the periphery which is engaged in the material varies with the topography of the workpiece.Would it be possible to provide an image of the actual cutter and collet?

[smarko77]

These are characteristics of the bit:
R0.75X20.5X4DX50L
But, it is not that. I did the same job with bit with 6mm diameter and these marks are shown on exactly the same spot.
What is best clue is that it is always shown on specific portions of the toolpath (between the letters). Like when machine have enough room to accelerate, instead of stoiping right before the edge of the letter, so it cannot accelerate same as when it just go through between the letter. Check my aspire toolpath preview picture what I mean.
I even tried to to raster on 90 degrees (meaning to use both X and Y axis) and same exact tool mark is shown. Maybe it has something to do with X and Y vs Z acceleration?

[MarkYu]

From what you've described, it seems that your CNC machine is producing irregular engraving marks when doing 3D engraving. This problem can be related to several factors. Here are some possible causes and solutions:

Acceleration and deceleration issues: You mentioned that the problem occurs in areas where the machine needs to slow down and cut intricate details. This may indicate that the machine's movement is not smooth enough during acceleration and deceleration, causing the tool to produce inconsistent engraving marks in these areas. You can try adjusting the acceleration and deceleration settings in Mach3, reducing the acceleration and deceleration values ​​to see if this improves the situation.

Stepper motor fine-tuning issues: Since you are using stepper motors, the low fine-tuning accuracy of stepper motors may cause inaccurate movement in specific areas, especially under high loads or deceleration. Try checking the motor's current settings to make sure they are appropriate for your application, and try increasing the current to improve the stability of the motor.

[smarko77]

MarkYu, seems that you solved my problem. When I increased acceleration, problem seems to be gone. I need to put it to more work to be sure, but I did same job twice with different acceleration configs and the one which had 5 times higher acceleration did the job much, much better. Perfect to be honest. Only problem I have now is that, because my gantry is really heavy, I get a lot of jerking motions which shake the whole table. I will try to play around and fine tune the best possible settings to avoid these shakes.
One question If I may. Is this Mach3 problem, or I would face the same issue with other software, like Mach4 or LinuxCNC? Seems to me strange that software itself doesn't have some mechanism to slow down one axis to match acceleration of another.